Using Surface Profile to control location combined with a size tolerance of feature (ISO1101)

[Brokenengineer]

Hi all,

I have a standard drawing note stating: 'Unspecified form to be within 0.2 surface profile of supplied CAD data.'
On a drawing of a sheet metal part, I have callouts for size control of holes, i.e. Dia. 5.3 +/- 0.05 mm

Is it correct to control the position on the sheet metal of the hole with the standard note surface profile, and then allow the size to be controlled with the specific callout?

Thanks,

 

[Belanger]

It would not correct to control the position on the sheet metal of the hole with the standard note surface profile because the note states "unspecified form" (emphasis added). It apparently doesn't give profile the power to control location.
But that does create an interesting situation where the size of the hole is allowed a total of 0.1 mm yet the form can be 0.2 mm. It seems to be a back-door independency situation, but somewhat strange if you ask me.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[Brokenengineer]

Thanks John-Paul,

Understood, but if the note were to say form and location?

Yes the idea is the hole size is important, its location less so. and to avoid basic dimensioning all the holes, to use the standard surface profile note to cover it?

thanks!

 

[Brokenengineer]

Is there a more appropriate way to get around having to locate each hole with basic dims and a TP call out?

 

[Burunduk]

You could specify a general note for position of holes and state that basic dimensions shall be queried from the cad model. You could have the following:

1. UOS ALL SURFACES |PROFILE|0.2|A|B|C|
2. UOS ALL HOLES |POSITION|Ø0.2(M)|A|B|C|
3. UNSPECIFIED DIMENSIONS ARE BASIC PER CAD DATA.

The diameters of the holes can be directly toleranced on the orthographic views or even stated in a general note if they are all the same (If you have several groups of holes, each with a different diameter, per ASME you could call them out with letters and use the note "INDICATED..." maybe there is a similar concept in ISO?).

It is always better to specify general controls with a datum reference frame that is functional for the application of the part.

 

[Burunduk]

It seems to be a back-door independency situation, but somewhat strange if you ask me.

The post title states ISO so independency is already in through the front door

 

[Brokenengineer]

Additional question:

Would it be acceptable to add a note to allow measurement of |PROFILE|0.2|A|B|C| with a +/-0,2 linear measurement on 'simple' features, for those companies who do not interpert GD&T / GPS.

 

[greenimi]

Would it be acceptable to add a note to allow measurement of |PROFILE|0.2|A|B|C| with a +/-0,2 linear measurement on 'simple' features, for those companies who do not interpert GD&T / GPS.

And in the case of the conflict which one would take precedence?
The profile ----|PROFILE|0.2|A|B|C|---- or the ± linear dimensioning method?

 

[Brokenengineer]

The Profile tolerance takes precedence. But i have QA at companies who do not interperate the GD&T correctly... at least the +/-0.2 linear is as close as you can get right?

 

[greenimi]

The Profile tolerance takes precedence.

So, if the profile takes precedence would you accept parts that are outside of the specified profile requirements because they qualified the parts per ±?

 

[Brokenengineer]

If they fit function on assembly, yes - its one of those catch all statements for people who do not interpret GD&T or dont have a CMM on hand so cant measure the parts. at least its a 'close enough' reference to thow a pair of calipers across the part.

for these parts, which are sheet metal... If they passed +/- 0.4 linear, but failed 0.4 profile, they will almost always fit function due to the ability to bend the part.

 

[greenimi]

If they fit function on assembly, yes.............

Therefore, if your acceptance criteria is "the parts fit the assembly" then you might NOT need a drawing with tolerances at all. Just try each and every part if they fit (or not the assembly)

 

[ctopher]

I prefer not to specify any type of GD&T in notes because it can be lost in translation, and misunderstood.
Add the callouts with the dimensions.

Chris, CSWP
SolidWorks '20
ctophers home
SolidWorks Legion

 

[greenimi]

....any type of GD&T in notes because it can be lost in translation, and misunderstood.

So then how would you handle the default profile tolerance, for example?
Your drawings do not have such as default profile (relativelly big tolerances for "unimportant" features) ?

 

[ctopher]

No. Each dwg calls out tolerances. We don't have default profile tolerances because each part is different. And, we don't use profile tol often; most parts are machined, square and straight. The dwg format has default tolerances. Example .XXX = +/-.003

Chris, CSWP
SolidWorks '20
ctophers home
SolidWorks Legion

 

[3DDave]

There used to be hard-gauge acceptance, which removes all the drawing dimensioning and tolerancing questions from the fabricator's hands. If it fits, it ships. If it doesn't fit, it's right there in front of the one who made the part to decide how to fix it.

 

[greenimi]

There used to be hard-gauge acceptance, which removes all the drawing dimensioning and tolerancing questions from the fabricator's hands. If it fits, it ships. If it doesn't fit, it's right there in front of the one who made the part to decide how to fix it.

Except that a hard gage does not fully qualify the part, just one side of the tolerance (talking about the profile one). The No-go validation with a hard gage is good for nothing as you cannot guarantee anything

 

[3DDave]

Don't tell the gauge makers.

It depends on how fully the part needs to be qualified. It sounds like a sloppy flexible sheet metal cover.

Not sure where you work, but the "other" side is checked with calipers, which appears to be the case here.

 

[Burunduk]

Would it be acceptable to add a note to allow measurement of |PROFILE|0.2|A|B|C| with a +/-0,2 linear measurement on 'simple' features, for those companies who do not interpert GD&T / GPS.

its one of those catch all statements for people who do not interpret GD&T or dont have a CMM on hand so cant measure the parts. at least its a 'close enough' reference to thow a pair of calipers across the part.

You need to choose between the two.
You can't have a geometric tolerance (for some suppliers) and a +/- tolerance (for other suppliers) on the same drawing to control the same characteristics of the same features, and letting the user choose which one he ignores.
They often have different meanings.
For example, if a profile tolerance applies to a hole or to opposing sides of a feature when it is specified all-around, 0.2 profile bares similarity to +/-0.2, but if one of the sides is datum feature A and has a flatness tolerance applied to it and the other side is controlled with profile within 0.2 relative to A (or A|B, or A|B|C), then the profile tolerance is like +/-0.1 (not +/-0.2) relative to the datum plane, and should be evaluated by a height gage, not a by a caliper.

Another problem is that you need basic dimensions for profile and dimensions stated without tolerance for the general +/- notation. If a note says that untoleranced dimensions are basic, the +/- tolerance doesn't apply to them. Maybe you can work around it, but to me, it is a bad idea anyway.

The biggest and most fundamental problem with a general +/- tolerance that a caliper can measure, is that it can only provide you a reliable evaluation of size. It cannot replace the general profile tolerance with a datum system as a tool that can control form, size, location, and orientation.